Guide
What straightness and exit position can deep hole drilling hold, and how should the drawing specify it?
Deep hole drilling is the making of a hole whose depth is many times its diameter, and the deeper the hole, the further its axis can drift from the line the drawing draws, so a hole that is on position at the entry face can break out off position at the far end. The reference overview of deep hole drilling, which draws on the VDI 3210 guideline on deep-hole methods, describes the drilling depth as usually greater than three times the diameter.
By Saola Manufacturing engineering team · Published · Updated
The complaint usually reaches engineering in one of three forms: a cross-drilled passage that does not meet the hole it was meant to intersect, a through hole whose exit sits outside the position tolerance even though the entry measured fine, or a long passage that breaks into a thin wall. None of these is fixed by asking the supplier to “hold it tighter.” Straightness and exit position depend on the drilling method, the depth-to-diameter ratio, the material and how the part is held, and most of those choices can be written on the drawing or the RFQ. This guide explains how to recognize drift, what causes it, how to measure it, which drilling method fits which depth, and how to dimension a long hole so the part can be made and checked without argument.
On this page
How do you recognize drill wander on a long hole?
Drill wander shows up as a hole whose entry is on position but whose exit, or whose intersection with another passage, is off. The size and finish at the entry often look perfect, which is why the problem is easy to miss at first-article inspection.
Typical signs on a received part:
- Exit off position. The breakout on the far face sits away from its nominal location, often more in one direction than another across a lot.
- Missed or partial intersections. A cross-drilled port meets the main passage with a step, a sliver, or not at all.
- Thin or broken walls. A passage running close to an outside surface bulges or breaks through partway along its length.
- Spiral marks in the bore. Mitsubishi Materials describes helical “rifling” marks on the hole wall as a symptom of wandering in its drilling accuracy course.
- A gauge pin that will not pass. A pin at the hole’s minimum size enters easily but binds partway down, even though bore-gauge readings of the diameter are in tolerance.
The geometry explains why the exit suffers most. The offset at the exit is roughly the position error at the entry, plus the hole depth multiplied by the tangent of the angle at which the drill started, plus whatever the drill bent along the way. A small angular error at the entry is invisible on the entry face and large at the far end of a long hole, so exit position is the feature to check when a long hole is suspected.
What causes a deep hole to drift off axis?
In rough order of how often they matter: a poor start at the entry, a drill that is too long, too slender or running out, chips and heat packing the flutes, and then material and setup effects such as hard spots, inclined surfaces and misalignment.
- Entry. A twist drill first touches the work with its chisel edge, which can skate before the lips engage. Mitsubishi Materials states that drilling a pilot hole with a stub drill first reduces wandering by 70 to 80% compared with no pilot, and recommends a pilot of 1 to 3 diameters deep (Mitsubishi Materials). An entry on a curved, inclined or as-cast surface makes skating worse.
- Tool runout and geometry. Sandvik Coromant advises that runout should not exceed 0.02 mm to achieve close hole tolerance and straightness with its solid carbide drills (Sandvik Coromant, how to use CoroDrill 460). Unequal lip heights after a regrind push the drill to one side; the same Mitsubishi course asks for a lip-height difference under 0.02 mm when regrinding.
- Misalignment. A Cutting Tool Engineering article notes that a drill that starts out of line, through misalignment of as little as 0.001 to 0.002 in or too much play in a guide bushing, produces a curved hole, and that the deeper the hole, the greater the deviation from the true axis (Cutting Tool Engineering, 1995).
- Chips and heat. The same article puts the critical depth for a simple twist drill at around four diameters as a rule of thumb, past which packed chips and heat stop it finishing in one pass, and reports 7 to 10 diameters without withdrawal for through-coolant versions. A drill forced through packed chips deflects; peck cycles, through-tool coolant and parabolic flutes all exist to prevent that.
- Feed and unsupported length. The same article warns that excessive feed can make a drill bend or spring, especially a small-diameter drill, and that a long drill may need a support bushing to limit side deflection. Halving the feed for the first diameter or two, and using the shortest drill that reaches, are the usual first trials.
- Material. Hard spots, inclusions, porosity in castings, and a hole that crosses another hole or a cavity all push the drill sideways where the cutting force becomes unbalanced. The CTE article notes that holes 8 to 10 diameters deep drill easily in free-cutting aluminum or brass, while some automotive forgings are difficult even at 2 diameters.
- Who rotates. Dedicated deep-hole machines can rotate the tool, the workpiece, or both in opposite directions; UNISIG describes counter-rotation as the arrangement preferred for closer tolerances (UNISIG). A hole off the axis of a rotating part, or in a prismatic block, can only be drilled with the tool rotating, so the workpiece-rotation and counter-rotation options are not available.
How deep can each drilling method go, and how straight will the hole be?
A standard twist drill is a short-hole tool, a parabolic or through-coolant drill reaches further with a pilot hole, and gun drills or BTA tools are the methods meant for long, straight holes. No method has a published standard straightness value, so treat any figure as a guide and agree the tolerance with the supplier.
The table below collects typical ranges from the sources listed at the end of this guide. Use it to judge whether a hole on your drawing is a routine drilling job or a deep-hole job before you choose the tolerance.
| Method | Typical depth or diameter range | Straightness behavior | Where it fits |
|---|---|---|---|
| Standard (jobber) twist drill | Critical depth around 4 × D in one pass; deeper with peck cycles, material dependent | Most sensitive to entry error, runout and chip packing | Short holes; long holes only with a pilot and pecking |
| Through-coolant or parabolic-flute twist drill | About 7 to 10 × D without withdrawal with through-coolant; parabolic flutes reduce the need to peck in some cases | Better chip flow; still follows the pilot it starts in | Medium-depth holes on machining centers and lathes |
| Stub-drill pilot, then long drill | Pilot 1 to 3 × D deep | Wander reduced by 70 to 80% versus no pilot | Any long twist-drilled hole |
| Gun drill (single-lip) | 0.5 to 40 mm diameter; to about 40 × D on machining centers; UNISIG suggests gun drilling from about 20:1 | Guided by pads on the bore wall; straightest with workpiece or counter-rotation, reported up to 0.08 mm per meter | Long small holes, hydraulic and coolant passages, shafts |
| BTA and ejector drilling | BTA 6 to 2000 mm diameter, industrial use from about 16 mm; ejector about 18 to 250 mm | Comparatively low straightness deviation; deep-hole methods generally reach IT9 to IT7 (ISO 286 grades), ejector drilling coarser | Large-diameter long bores on dedicated machines |
Two cautions apply when reading those figures. First, the best gun-drilling straightness quoted by machine builders assumes a dedicated machine with counter-rotation; UNISIG cites up to 0.08 mm per meter for that arrangement (UNISIG), and the same article notes that retrofitting gun drilling onto an existing machine is effective only to about a 10:1 ratio. Second, even that best-case figure is not zero: on a 500 mm passage it allows about 0.04 mm of drift by the same UNISIG figure, which is already larger than many position tolerances drawn by habit. When a drawing asks for a long hole to hold the same position at the exit as at the entry, the drawing is usually asking for more than the method can promise.
How do you measure straightness and exit position on a deep hole?
Measure the hole at both ends, not only at the entry: position at the entry face and at the exit face against the same datums tells you where the axis went. For straightness of the axis, use a functional gauge pin at virtual condition or a coordinate measuring machine that probes the bore at several depths.
- Entry and exit position. Measure the center of the hole on each face against the drawing datums. The difference between the two, divided by the depth, is the angular error of the axis; a constant offset at both ends points to setup, while a growing offset points to drift.
- Functional gauge pin. When straightness of the derived median line is specified at maximum material condition, a fixed pin at the virtual condition size, the maximum material size minus the straightness tolerance per ASME Y14.5, must pass the full depth of the hole. The MMC bonus tolerance guide explains why that gauge works.
- CMM scanning at several depths. Probing circles at intervals along the bore and constructing the axis gives straightness and position over the full length, but only as deep as the stylus can reach; the CMM inspection guide covers what to ask for in the report.
- Wall thickness checks. Where a passage runs close to an outside surface, an ultrasonic thickness reading along the length shows whether the drill drifted toward the wall without cutting the part.
- Sectioning at first article. For a new or difficult hole, cutting one part through the passage is the most direct proof of where the axis went. Agree in advance that one part is sacrificed.
Write the measurement method on the purchase order. “Position checked at entry and exit faces” and “gauge pin at virtual condition through full depth” are short notes that remove most disputes about whether a long hole passed.
How do you fix or prevent a wandering deep hole?
First decide whether the problem is the process or the drawing. If the hole is within a sensible depth for its method, fix the start, the tool and the chip evacuation; if it is not, change the drilling method or change the design so the hole is shorter or its exit tolerance is wider.
| Symptom | Most likely cause | Process fix | Drawing or design fix |
|---|---|---|---|
| Entry already off position | Drill skating on the surface; no spot or pilot | Spot or stub-drill pilot; flat entry face | Add a spotface or flat where the drill enters an inclined or cast surface |
| Entry on position, exit off in one direction | Angular start: runout, misalignment, uneven lip heights | Check tool runout and regrind quality; guide bushing | Specify exit position separately, or allow a wider zone at the exit |
| Exit off in random directions across a lot | Deflection from chip packing or long slender drill | Peck cycle, through-tool coolant, lower feed, shortest drill or a support bushing; parabolic or gun drill | Shorten the hole; drill from both ends |
| Drift near cross holes or cavities | Unbalanced cut where the drill breaks into another feature | Drill the long hole first; reduce feed through the intersection | Move the crossing or enlarge the intersecting hole |
| Breakout into a thin wall | Normal drift on a hole placed too close to a surface | Gun drill with workpiece rotation where the part allows | Increase wall stock along the full length |
| Varies lot to lot with the same program | Material lot, regrind practice or coolant condition | Control regrind and runout; record material heat | Name material and condition; require first-article sectioning |
The design fixes are often cheaper than the process fixes. A long passage that only has to carry fluid can be drilled from both ends to meet in the middle, with an allowed step at the junction, instead of being drilled through from one side. A passage that has to turn a corner is usually made as two or more straight drillings that intersect, with the unwanted openings closed by plugs; in that case the drawing should show the plug, its sealing requirement and the minimum overlap of the intersecting holes, rather than a position tolerance that tries to force the drills to meet exactly. A reamer, as the reamed vs drilled hole guide explains, sizes and finishes a hole but largely follows the hole it is given, so it does not correct a drifted axis.
How should the drawing and RFQ specify a deep hole?
Control the hole with position at maximum material condition over the depth that matters, add straightness of the derived median line only if the function needs it, and say how the exit or the intersection will be checked. Then tell the supplier on the RFQ which of those controls are functional and which can be relaxed.
Under ASME Y14.5, a position tolerance on a hole controls its axis over the full length of the feature, so a single position callout already limits how far the exit can wander. Straightness applied to the size of the hole controls the form of its derived median line but not its location; the straightness guide explains the difference. The drawing checklist for a long hole:
- State depth and through or blind. Give the full depth and the diameter so the depth-to-diameter ratio is obvious at quoting.
- Position at MMC. Use position at maximum material condition so a hole drilled larger gains bonus tolerance and a functional gauge can be used.
- Different requirements at entry and exit, if the function allows. Where only the entry has to locate a fitting, apply the tight position to a limited length at the entry, using the limited-length indication in ASME Y14.5, and give the remainder a wider zone.
- Intersections by overlap, not by position. For drilled passages, state the minimum overlap or flow area where holes meet, and show plugs and their sealing test.
- Allowed manufacturing alternatives. Say whether drilling from both ends is acceptable and what step is allowed at the junction.
- Inspection method. Name entry and exit position checks, a gauge pin at virtual condition, or CMM probing at several depths.
- Material and condition. Name the grade and condition; a free-cutting grade and a tough alloy do not drill the same way.
On the RFQ, add one line explaining what the hole does, for example “coolant passage, only sealing and flow matter” or “guides a pin at the exit face.” That sentence lets the supplier propose drilling from both ends, a plug, or a wider exit tolerance before quoting a dedicated deep-hole process the part does not need, and it is the cheapest way to avoid paying for straightness the function never uses. The design for machining guide lists other features worth questioning at the same time.
How is a deep hole handled on a Saola order?
Long holes in machined parts are drilled at our lead CNC plant, T.K Viet Nam Precision Company Limited, on CNC lathes for holes on the part axis and on machining centers for holes off it. If a hole needs a dedicated deep-hole process, the quote says so and names where it will be made.
Holes on the axis of a turned part are drilled on center with the part rotating, as described on the CNC turning page, while cross holes and passages in blocks and housings are drilled on machining centers, as described on the CNC milling page. The published equipment list for the lead CNC plant does not include a dedicated gun-drilling or BTA machine, so when the depth-to-diameter ratio on your drawing calls for one, our engineers will either propose a design alternative such as drilling from both ends, or state on the quote how and where the hole will be made. Inspection equipment at the plant includes a 2D vision measuring machine and a height gauge; if your hole needs a CMM report or a functional gauge, name it on the RFQ and the quote will state how it is verified. When the long hole is in a casting, the casting comes from a partner plant we manage and is then machined, and each quote names the production site and the country of origin. ISO 9001 certification is in progress, not held. Send the drawing, with the function of the hole in one line, through the quote form.
Frequently asked
What depth-to-diameter ratio counts as a deep hole?
There is no single cutoff. The deep-hole literature summarized from VDI 3210 usually starts deep-hole work at depths greater than three diameters, while trade guidance puts the limit for a standard twist drill in one pass at around four diameters. Beyond that, expect peck cycles, longer drills, a pilot hole or a gun drill.
Is drilling from both ends an acceptable way to make a long hole?
Often, yes, for passages that carry fluid or clear a part. The two drillings will not meet perfectly, so the drawing should allow a step or mismatch at the junction and state the minimum open area. It is not suitable where a pin or shaft has to slide the full length of the hole.
Will reaming or honing straighten a drifted hole?
Not reliably. A reamer follows the existing hole and improves size and finish, and honing improves form and finish over the length. Neither moves the hole back to its nominal location, so a drifted exit has to be fixed in drilling or allowed by the drawing.
Does a straightness callout control where the hole exits?
No. Straightness of the derived median line controls the form of the axis only. Where the hole exits relative to the datums is controlled by position, which applies to the whole length of the hole, so check position at the exit face if the exit matters.
Why are some lots straight and others not, with the same program?
Look at what changed between lots: material heat and hardness, drill regrinds with unequal lip heights, tool runout in a new holder, or coolant concentration and pressure. Recording the material heat and the tool used for each lot makes the cause easy to find.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018
- ISO 1101:2017, GPS — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017
- ISO 286-1:2010, GPS — ISO code system for tolerances on linear sizes — Part 1, ISO, 2010
- VDI 3210 Blatt 1, Deep-hole boring (scope), VDI, 2006
- Deep hole drilling (overview citing VDI 3210 and the deep-hole drilling literature), Wikipedia, accessed October 2026
- Deep Thoughts: Drilling Performance (R. Moring), Cutting Tool Engineering, 1995
- Gunning for Better Results (A. Fettig), UNISIG, 2012
- Drilling accuracy and quality, Mitsubishi Materials, accessed October 2026
- How to use CoroDrill 460, Sandvik Coromant, accessed October 2026